J2.2
DEVELOPMENT AND APPLICATIONS OF CFD SIMULATIONS IN SUPPORT
OF AIR QUALITY STUDIES INVOLVING BUILDINGS
EPA/600/A-04/078
*1Alan Huber
Atmospheric Sciences Modeling Division, ARL/NOAA, RTP, NC
1 on assignment to National Exposure Research Laboratory, US EPA, RTP, NC
Wei Tang
National Research Council Research Associate at National Exposure Research Laboratory, US EPA, RTP, NC
Anita Flowe
Independent Contractor, Roxboro, NC
and
Brian Bell, Karl Kuehlert, and Walter Schwarz
Fluent Inc, Lebanon, NH
1. INTRODUCTION
There is a need to properly develop the
application of Computational Fluid Dynamics (CFD)
methods in support of air quality studies involving
pollution sources near buildings at industrial sites.
CFD models are emerging as a promising technology
for such assessments, in part due to the advancing
power of computational hardware and software. CFD
simulations have the potential to yield more accurate
solutions than other methodologies because they are
a solution of the fundamental physics equations and
includes the effects of detailed three-dimensional
geometry and local environmental conditions.
However, the tools are not well validated for
environmental flows and best-practice methodologies
have not been established. Fluent, Inc and the US
EPA National Exposure Research Laboratory are
working cooperatively to demonstrate CFD model
simulations as a proven and applied tool in support of
environmental assessment studies. See also Huber
et al 2000a, 2000b, and 2001 for additional
perspectives related to this project.
The results of CFD simulations can both be
directly used to better understand specific case
studies as well as be used to support the
development of better-simplified algorithms that may
be generally applied. Unlike most currently used
regulatory air quality models, CFD simulations are
able to include specific details of building structures
as well as a range of physical processes that affect
atmospheric turbulent boundary layers. Dispersion in
absence of buildings is demonstrated in this paper to
be comparable with standard plume dispersion
models for point and line source pollutant emissions.
Boundary layer turbulence is being simulated as
characterized by surface roughness (characterized by
* Corresponding author address: Alan H Huber,
NOAA/ERL/ARL/AMD, Mail-Code E243-03, US EPA
NERL, RTP, NC 27711
e-mail: huber.alan@epa.com
u*) and surface heat flux (characterized by the
Obukhov length L).
This paper discusses ongoing development and
application of CFD simulations through case studies
using CFD software for simulating air pollutant
concentrations from sources near buildings.
Comparisons of CFD simulations to reference wind
tunnel data and field measurement studies are being
studied to provide model evaluation/validation. CFD
simulations should be shown to be comparable with
simple proven air dispersion models being reliably
applied today in routine air quality studies. This is
critical to demonstrate that the complex numerical
techniques that are part of CFD software are well
behaved under simple conditions. We do not need
CFD software to support studies where simple
analytical solutions are possible. We do want to
extend CFD applications for complex conditions
where we know simple analytical solutions are not
appropriate. While we have already explored many of
the basic elements of CFD software there is much
ongoing that needs to be completed before we make
recommendations. An overview on progress with our
evaluation and development of CFD applications
appropriate in supporting of air quality studies
involving buildings is presented herein.
2. CFD SOFTWARE
A brief overview of the numerical methods is
provided here. The discussion is meant only to
present an introduction for someone that may be new
to CFD software. CFD software involves many layers
of coding with complex interactions. For this reason
any CFD software should be carefully examined and
have a history of quality assurance testing before one
begins to apply it to support air quality studies.
Those interested in additional introductory reading on
CFD issues can find many good reference books (for
example: Ferziger and Peric, 1997; Wesseling, 2000;
and Wilcox, 1998)

-------
The FLUENT software (Fluent Inc, 2003) solves
the governing equations for the conservation of mass,
momentum, energy, and scalars such as a pollutant.
The study domain is divided into discrete control
volume cells using a computational grid mesh.
Unstructured meshing supports variable volume cell
sizes throughout the domain. This allows for better
computational efficiencies by being able to
concentrate the grid mesh in areas where finer mesh
is most critical in resolving complex flows. Algebraic
equations for discrete dependent variables such as
velocities and pollutants are constructed and solved.
There are options for both a coupled equation solver
using either an implicit and explicit discretization, or a
segregated equation solver having implicit
discretization.
For atmospheric flows the segregated solver using
implicit discretization is appropriate and is being used
for our studies. The momentum equations are solved,
and then a pressure-correction is applied to update
the pressure field to support calculation of mass
fluxes to ensure conservation of mass. The solutions
for energy, turbulence and other scalar equations
(i.e., pollutants) follow separately. In the implicit
discretization for a given variable the unknown value
in each cell represented at the cell center is
calculated using both existing and unknown values
from neighboring cells. Overall the software uses an
algebraic multigrid method to solve the resultant
system of equations for the dependant variable in
each cell. The calculations continue and update all
the cell properties until selected criteria for a
converged solution is reached. There are options for
obtaining volume face values by applying first-order,
second-order, power-law, and for quadrilateral/
hexahedral grid mesh the QUICK (Quadratic
Upstream Interpolation for Convective Kinematics)
scheme. There are specific options for pressure
interpolation including linear, second-order, body-
force-weighted, and PRESTO (PREssure Staggering
Option). For pressure-velocity coupling the options
are SIMPLE (Semi-Implicit Method for Pressure-
Linked Equations), SIMPLEC, and PISO (Pressure-
Implicit with Splitting of Operators). We have not
noticed a significant effect among these different
choices for our simulations to date.
The software has options for either steady or
unsteady (time-varying) solutions. There are options
for a first order and higher order implicit schemes for
temporal discretization of the time derivative. To date
we have not been examining unsteady flow solutions.
We have started with the simplest applicable CFD
models for supporting air quality studies involving
buildings. We have been evaluating solutions for the
Reynolds-Averaged Navier-Stokes (RANS) governing
equations for momentum. Solutions require a
selection of boundary conditions and a model for
turbulence. The software has options for the wall
(ground surface) boundary conditions and several
turbulence models. We have been evaluating the
performance of standard k-e (turbulent kinetic energy:
k; turbulent energy dissipation rate: e, epsilon)
turbulence model. This is our base case. In the
future we plan to examine higher order turbulence
closure models including Reynolds Stress Models
(RSM) and Large Eddy Simulation (LES) along within
the framework of unsteady solutions. The
computational requirements of these higher order
solutions may not be practical for support of routine
air quality studies but may be useful for special cases
studies where detailed analyses of pollutant
dispersion is important in human exposures. Also,
higher order simulations may support the
development of reliable simplified models of human
exposures to pollution.
3. AMOSPHERHIC BOUNDARY LAYER AND
PLUME DISPERSION
Simulation of the atmospheric boundary layer is
critical to modeling plume dispersion. While the
primary interest in application of CFD methods is to
simulate flow around buildings the CFD code should
first be demonstrated to correctly model a plume in
absence of any buildings. The CFD simulated flow
should be simple and well defined in absence of
building influences. If there are problems within the
CFD code they can be more easily identified. Flat
plate and atmospheric boundary layer theory provides
a basis for testing the sensitivity of CFD code
parameters over a range of boundary conditions.
Monin-Obukhov similarity theory is applicable to
atmospheric boundary layers. For CFD simulations a
surface heat flux (H, W/m2) is fixed as the bottom
boundary condition to simulate non-neutral stability
conditions. The CFD boundary layer flow is set up by
using a finely resolved grid with application of the "law
of the wall" near the bottom. The surface friction
velocity (u*) is estimated from the resulting wind
profile. Figure 1 presents example profiles of mean
streamwise velocity and temperature with and without
added heat flux. Figure 2 presents a summary of
simulated Obukhov length (L, m) versus surface
friction velocity that result from a range of simulations.
These results are found to compare well with Monin-
Obukhov theory (see Figure 11.1, Arya 2001).
Simulation of pollutant plume dispersion requires
good models for both the bulk transport and the
turbulent dispersion of the pollutant. Good simulation
of the bulk transport is expected if the mean flow field
is correctly modeled. Good turbulent dispersion
requires that the turbulent flow be correctly modeled.
For this study we are only evaluating RANS
simulations and using several k-e turbulence models,
which produces turbulent kinetic energy (TKE) driving
turbulent pollutant dispersion. Dispersion from line
and point sources are being studied to evaluate the
performance of the turbulence models. The standard
turbulence model has been generally working well
using standard code default parameters for simple

-------

14

12

10
U)

E
8
>

o
6
o


4

2

0
-velocity, heat flux = 200W/mA2
-velocity, no heat flux
^temperature, heat flux = 200W/mA2
292
291
290
289
288
3
TO

c
o
_l
>
o
3
•fi
O
10
1
—400W/mA2
—300W/mA2
-*-200W/mA2
100W/mA2
—40W/mA2


t
/

0.01
10
m/s
0.1	1
Friction Velocity, u*
Figure 2. Monin-Obukhov theory applied to a range
of case studies.
flows. Some additional evaluations and refinements
are ongoing to improve performance, especially for
highly buoyant cases. No work has yet been started
to evaluate strongly stable stratified flow. Figure 3
presents a comparison with a line source assuming
P-G Gaussian plume urban dispersion parameters
(Stability C). The concentrations are normalized by
the wind speed at 10 m (u, m/s) and the source
strength (q, gm/s).
Matching both the full lateral and full vertical
profiles of the plume beyond the centerline present
challenges which are being examined in more detail
than can be covered in this presentation. The CFD
simulations include effects of wind shear and
characteristics of the turbulence model that must be
more carefully evaluated. While plume centerline
peak concentrations are of primary interest in air
quality studies, when the study includes a series of
ranging wind directions the location of overall peak
concentrations can be altered significantly by off-
centerline concentrations. Also, peak concentrations
near the ground can be significantly altered by off
centerline plume concentrations for elevated sources.
1.0E+00 -
	heat flux = 200W/mA2, U100m
= 3.0m/s Ri =
-0.94
	heat flux = 400W/mA2, U100m
= 7.9m/s Ri =
-0.19
urban line source


— 1.0E-01
o 1-0E-02
w 1.0E-03
E
1.0E-04
1.0E+01	1.0E+02	1.0E+03
Distance from source, m
1.0E+04
Figure 3. Comparison of normalized concentrations
(Cu/q, m"2) with urban P-G line source.
4. PROJECT PRAIRIE GRASS SIMULATION
Field measurements in the atmospheric boundary
layer contain inherent variability due to unsteady
winds that are case specific. This factor is not fully
captured by the simple Gaussian straight-line plume
formulations. Development of Gaussian straight-line
plume models in regulatory use has been formed, in
part, on an early field study, Project Prairie Grass
(Barad, 1958). Field measurements from this study
are being used to evaluate methods for direct
application of CFD simulations of specific cases for
simple atmospheric flows. For these case studies
there are ranges of wind directions that are not part of
the steady-state RANS CFD simulations.
We are working with these field measurements to
evaluate methods for the best CFD simulations of all
measurements for each case. Methods include
accounting for variation in wind direction by
smoothing the steady solution over the wind
distribution or by enhancing the lateral dispersion
internally. Figure 4 presents an example simulation
for one case having minimal wind variation (Case 55,
Barad 1958). In the figure for each of 4 distances
downstream from the near ground source the CFD
simulation is compared with the field measurements,
routine P-G (stability D) straight-line plume estimates,
and the CFD solution weighted by

-------
a) Arc distance = 100 m
5 4
!¦

— CFD-weighted

• measurements

— CFD

plume model


•
• 1
L
¦»1





W*.
320
330	340
Direction, degrees
b) Arc distance = 200 m

i CFD-weighted

• measurements

	 CFD

—» plume model
•


1
• I

• A

A
IV

-A v
f/T


N •
320	330	340
Direction, degrees
c) Arc distance = 400 m
5 4

— CFD-weighted

• measurements

— CFD

plume model
J

1 * I
• |

If
¦J
A-
-y\

lv\

yV.
310
320
330	340
Direction, degrees
d) Arc distance = 800 m
4.5
4
3.5
i 3
£
S 25

— CFD-weighted

• measurements

	CFD

.... plume model
ml

m

• f •

Jr

A
ft
JJr
-.v\
¦ .rii

330	340
Direction, degrees
Figure 4, Example Prairie Grass case.
the distribution in wind direction as a smoothing
function. The CFD simulation was matched to the
measured vertical profile of wind speed from 2 m to
16 m with a friction velocity u*=0.44 m/s and
roughness height zO = 0.009m.
Similar results are being observed for other cases.
It appears that the measurements lie between the
default steady-state RANS simulation and these
simulations smoothed over a function of the wind
direction. Best methods will be developed based on
the whole database. While the Project Prairie Grass
is an especially good database for examining the
horizontal plume it has only a few vertical plume
profiles. Additional field measurements including
more vertical profiles are desirable. There are few
vertical profiles because they are naturally more
challenging to collect. Additional databases for better
examining the vertical plume profiles are being
searched. The preliminary CFD simulations of flow
and dispersion for an atmosphere-like boundary layer
has been determined sufficient to begin applications
to areas with buildings.
5. BUILDING SIMULATIONS
Fortunately there are many databases on flow
near buildings from scaled physical model studies in
wind and water tunnels. The boundary layers are
simple without many of the chaotic and complicating
factors in actual field situations. Simple idealized
buildings can be systematically studied. These data
are ideal for evaluating the performance of CFD
models because boundary conditions are well
controlled. CFD models should be demonstrated to
simulate the scaled model studies before moving
forward to full-scale field situations. These
simulations should help identify potential errors in
model coding or identify limitations of physical
models.
Data from studies conducted in the US EPA's
Meteorological wind tunnel are being used to initially
evaluate CFD code for our project. This EPA wind
tunnel study (Lawson et al, 2000) was conducted in
collaboration with the Los Alamos National Laboratory
and the Lawrence Livermore National Laboratory. The
study included measurements of velocity and tracer
concentrations within arrays of two-dimensional (2D)
and three-dimensional (3D) buildings. These data are
being used by others to evaluate other model
performance (Brown et al.. 2000; Chan et al., 2000;
Kastner-Klein et al, 2000). The buildings for the 2D
study were set with seven square cross sections
spanning the width of the wind tunnel. The separation
between the buildings was equal to the cross-section
building scale (0.15 m). The buildings for the 3D
study covered the same area as that for the 2D study
but consisted of cubes separated by open space of
the same volume as each cube.

-------
For these studies the wind tunnel ceiling was
adjusted to reduce the horizontal pressure gradient.
Three triangular fins (spires) at the inlet and 0.19 mm
blocks on the floor were used to develop a 165 m
deep wind tunnel boundary layer. The roughness
blocks are absent on the floor in the study area with
the model buildings. The CFD simulations begin by
developing a set up trying to match the wind tunnel
boundary layer at the inlet. The wind tunnel
measurements of mean velocity can be matched at
the inlet well as long as the velocity profile is set
correctly. Matching the TKE field requires a good
estimate of the dissipation rate, for which there are no
direct measurements.
Figures 5 and 6 present comparisons of the
measured (green) with the CFD (black) velocity
vectors near the leading two rows of buildings. The
coordinate origin (x=0, y=o, z=0) is located at the
base of the leading building (cross-stream center of
the leading building. The region in front of the leading
building and over its roof has the greatest difference
in the flow field between 2D versus 3D and is the
most challenging to CFD simulation because of the
small regions of recirculation flow. The CFD
simulations resulted from using standard default set
up. The grid resolution was with 30 cells per building
face. Studies of grid resolution demonstrated grid
independence at this fine scale. The measured flows
were very similar and well matched for the flow over
the roof and street canyons between rows 3 to last
row 7. Figure 7 presents comparisons for a vertical
profile in the first building street canyon (between
building 1 and 2). Included are simulation profiles at
the same location without the buildings. The CFD
simulations resulted from default set up parameters.
The mean velocities both with and without buildings
are well matched with the measurements. The TKE
without buildings is well matched except for the near
wall zone. The TKE profiles with buildings are similar
to measures but too low in a near wall zone and too
high in the upper zone.
The wind tunnel study with the 3D buildings
includes an examination of tracer dispersion from a
source placed at the leeward base of the first building
(x=0.15, y=0). Figures 8 and 9 present example
comparisons between the measurements and the
CFD simulations using the standard default set up.
Concentrations gradients in the first (source
containing) street canyon are greatest and are well
matched by the CFD simulation. The comparisons are
likewise good in the second street canyon (as well as
the other street canyons not shown) where the
gradients are greatly reduced due to the uniform
mixing imposed by the flow through the streets.
These comparisons demonstrate that with good
simulations of the mean flow even without matching
TKE, the transport and dispersion of tracer
concentration in street canyons can be matched.
Profiles of velocity and concentrations are more
complex and have more complex gradients in the
along-stream street canyons. Further examinations
are ongoing for more complex building street canyon
studies.
Modifications to the standard default CFD set up
are being examined to identify how best to improve
the simulations of TKE for this study. These include
assessing performance of different turbulence
models, boundary conditions (especially inlet and
top), surface wall models, and grid resolution. Some
preliminary comparisons are presented in Figures 10
and 11 near the leading 2-D building where
differences have been most noticeable. Figure 10
shows how blockage effects that were observed for
the 2-D case study can significantly affect the flow in
front of the leading 2-D building. The roof in the wind
tunnel is adjusted to minimize horizontal pressure
gradients in the free-stream flow. Therefore having
the correct ceiling boundary condition is critical. Also,
further improvements in the CFD simulations are
possible when dissipation rate (e - epsilon) is better
estimated. Refined simulations of the wind tunnel
boundary layer development are providing significant
improvement as presented in Figure 10. In Figure 11
the present simulations show that TKE over the roof
of the leading 2-D building is not significantly affected
by the ceiling boundary conditions but is significantly
affected by inlet dissipation rate,
Black=FLUENT
Green=Wind tunnel
Reference, m/s
J—
CD
"S
£
c
*-»
.c
o>
"a>
I
0.3-r
0.2-
0.1-
Iff!
fi! if if!
$3 J
I
-0.1
0 0.1 0.2 0.3 0.4 0.5
Streamwise distance in meters
Figure 5. Velocity near two-dimensional buildings.
0.6
Black=FLUENT
Green=Wind tunnel
Reference, m/s
o" 3H
0 0.1 0.2 0.3 0.4 0.5
Streamwise distance in meters
Figure 6. Velocity near three-dimensional buildings.

-------
a) Mean Velocity (m/s)

2 —
— — — FLUENT 2-0 flat plate
	 FLUENT 2-D with buildings
	FLUENT 3-0 flat plate
FLUENT 3-0 with buildings
•	# • Experimental 3-D with buildings
•	+ • Experimental 2-0 with buildings
9 • # Experimental flat plate
"i	¦—i	1	1	1	1	1	1
-2	0	2	4	6
Streamwise velocity in meters
0.1 0.15 0.2 0.25 0.3 0.35 0.4 0.45 0.5 0.55 O.f
Streamwise distance in meters
Figure 8. Concentrations within 3-D building canyons
at y=0 (CFD color contour, Wind tunnel data
numbers).

III;
Wind tunnel x=O S25
FLUENT x=0.525
Wind tunnel x=0.225
FLUENT x =0.225
-0-2	O	0.2
Cross-stream, meters
c) Turbulent Dissipation (m Is
	— FLUENT 2-0 flat plate
	FLUENT 2-0 with buildings
	FLUENT 3-0 flat plate
	FLUENT 3-0 with buildings
—I	1 I II II11' I ¦ I ¦ I l 11|	1	1 I l 1 II l|
0.01	0,1	1	10
Turbulent dissipation mA3/sA3
Figure 9. Cross-stream concentration profiles with 1s
building canyon (x=0.225) and 2"" building canyon
(x=0.525).
s
<
£
UJ
Figure 7. Profiles within the first building canyon.
Figure 10. Turbulent kinetic energy in front of leading
2-D building face (x=~0.038 m, y=0).
b) Turbulent Kinetic Energy (m Is
2.5 -i
	FLUENT 2-D flat plate
	 FLUENT 2-D with bu i Idings
	FLUENT 3-D flat ptale
FLUENT 3-D with buildings
•	• $ Experimental 3-D with buildings
•	9 9 Experimental 2-D with buildings
9 • Experimental flat plate
r
0.4	0.8
TKE in m*2/sA2
	 Ceiling BC, estimated dissipation
	 Ceiling BC. spires simulation
9 # t Wind tunnel data
- Symmetry BC, estimated dissipation
0.1 0.2 0.3 0.4
Vertical position in meters

-------
2.5 -i
2 -
(M
JS 1.5
(M
<
£
LU
*
1 "
0.5 -
—T	1	1	1	1	T"
0.1	0.2	0.3	0.4
Vertical distance in meters
0.5
Figure 11. Turbulent kinetic energy on leading 2-D
building roof edge (x=0.045 m, y=0).
6. OVERVIEW
Much is being learned about how best to set up
CFD simulations to support environmental simulations
and the issues that most affect comparability with
both physical model studies and field measurement
studies. The choice of boundary conditions, grid
resolution and structure, and turbulence models affect
the outcome of a solution significantly. Transport and
dispersion can be well simulated for flat plate
boundary layers as used in physical model studies.
Transport and dispersion simulations are more
complicated for atmospheric flows due to the complex
temporal-spatial wind fluctuations.
To date the project has focused on RANS steady-
state solutions and the standard k-e turbulence
models. This is being extended to include unsteady
solutions and higher order turbulence models.
Detailed technical papers will be prepared as this
project reaches significant conclusions.
REFERENCES:
Arya, S. Pal, 2001: Introduction to micrometeorology.
2nd Edition. Academic Press, San Diego CA.
Barad, M.L. (Editor), 1958: Project Prairie Grass, A
Field Program in Diffusion. Geophysical Research
Paper, No. 59, Vol I and II, Report AFCRF-TR-58-
235, Air Force Cambridge Research Center,
Bedford, MA.
Brown, M., R. Lawson, D. Descroix, and R. Lee,
2000: Mean flow and turbulence measurements
around an array of buildings in a wind tunnel. 11th
AMS Conference on Applications of Air Pollution
Meteorology. January, Long Beach, CA.
Chan, S.T., D. Stevens, and R. Lee, 2000: A model
for flow and dispersion around buildings and its
validation using laboratory measurements. Proc. 3rd
AMS Symposium on the Urban Environment, 14-18
August, Davis, CA., 56-57.
Ferziger, J. and M. Peric 1997: Computational
Methods for Fluid Dynamics. ISBN 3540594345.
Springer-Verlag, New York. 364 p
Fluent, Inc 2003: FLUENT 6.1 User's Guide. Fluent
Inc, Lebanon, NH.
Huber, A., S. Rida, E. Bish, and K. Kuehlert, 2000a:
Addressing Environmental Engineering Challenges
with Computational Fluid Dynamics. Proceedings of
the 93rd Annual Meeting of the Air & Waste
Management Association, June 18-22, 2000, Salt
Lake City, UT. Air & Waste Management
Association, Pittsburgh, Paper No. 1073.
Huber, A., Bolstad, M. Freeman, S. Rida, E. Bish, and
K. Kuehlert, 2000b: Addressing human exposures to
air pollutants around buildings in urban areas with
computational fluid dynamics (CFD) models, 3rd
Symposium on the Urban Environment, 14-18
August, Davis, CA., 62-63.
Huber, A, M. Freeman, S. Rida, K. Kuehlert, and E.
Bish, 2001: Development and Applications of CFD
in Support of Air Quality Studies of Roadway and
Building Microenvironments. Proceedings of the
94th Annual Meeting of the Air & Waste
Management Association, Orlando, Florida, June
24-28,2001. (CD-ROM). Air & Waste Management
Association, Pittsburgh, Paper No. 1035.
Kastner-Klein, P., M. Rotach, M. Brown, E.
Fedorovich, and R. Lawson, 2000: Spatial
variability of mean flow and turbulence fields in
street canyons. Proc. 3rd AMS Symposium on the
Urban Environment, 14-18 August, Davis, CA, 13-
14.
Lawson, R., S. Perry, and R. Thompson 2000:
Measurement of Velocity and Concentration Fields
in Arrays of 2-dimensional and 3-dimensional
Buildings in a Simulated Neutrally-Buoyant
Atmospheric Boundary Layer, U.S. EPA, RTP, NC,
55 pp.
Wesseling, P., 2000: Principals of Computational
Fluid Dynamics. ISBN 3540678530. Springer-
Verlag, New York. 642 p.
Wilcox, D., 1998: Turbulence Modeling for CFD.
ISBN 0963605151. DCW Industries, La Canada,
CA. 540 p.
ACKOWLEGMENT: Appreciation is extended to Dr
Steven Perry and Dr David Heist of the US EPA Fluid
Modeling Facility for their advice and assistance in
understanding the wind tunnel model studies.
	 Ceiling BC, estimated dissipation
- Ceiling BC, spires dissipation
9 # • Wind tunnel data
Symmetry BC, estimated dissipation

-------
Disclaimer: The research presented here was
performed under the Memorandum of Understanding
between the U.S. Environmental Protection Agency
(EPA) and the U.S. Department of Commerce's
National Oceanic and Atmospheric Administration
(NOAA) and under agreement number DW13921548.
Although it has been reviewed by EPA and NOAA
and approved for publication, it does not necessarily
reflect their policies or views.

-------